Newbie check

[jbelle7435]

Attached is my MC file and below is the code from the file.

 

%
O0001(01B _HOLE)
(DATE=DD-MM-YY - 19-09-13 TIME=HH:MM - 16:01)
(MCX FILE - Y:\PB\MASTERCAM\REFERENCE\01A_HOLE.MCX)
(NC FILE - Y:\PB\MASTERCAM\REFERENCE\01B _HOLE.NC)
N100 G0 G20 G90
N110 G92 X0. Y0. I1. J0.
N120 G0 X0. Y0.
N130 M60
N140 M35
N150 M81
N160 S101 D1
N170 G41 G1 X.32322 Y-.32322
N180 G2 X.5 Y-.25 I.17678 J-.17678
N190 X.75 Y-.5 J-.25
N200 X.5 Y-.75 I-.25
N210 X.25 Y-.5 J.25
N220 X.32322 Y-.32322 I.25
N230 G40 G1 X0. Y0.
N240 M50
N250 M30
%

 

My concern is I been using MC for about less than a week along with help from Youtube/PDFs Tutorials. Is this part ready to be made(hole cutout) on a WEDM? If there any concerns beyond that let me know so I can better myself from this point foward? We use a : "Mitsubishi 1990: HA Series" http://www.mitsubish...58&Itemid=1158.

 

Hope soon I can be importing CAD models and setting them up properly for machining with MC.

01B_HOLE.MCX

[Del.]

If you are cutting the hole to .5 dia. i think it should be G42 instead of G41.

 

 

I don't use Auto comp but choose either left or right.

[jbelle7435]

If you are cutting the hole to .5 dia. i think it should be G42 instead of G41.

 

 

I don't use Auto comp but choose either left or right.

 

I know the internet is not always right but I found:

 

G41 means the cutter stays to the left of the programmed path.

G42 means the cutter stays to the right of the programmed path.

 

If this is true with WEDM as well, is it not that important knowing the tolerance is pretty small so I should still get my .5 dia hole within or am I losing my case?? I know for a tool(mill) it might be more relevant(left, right)...

[Del.]

I know the internet is not always right but I found:

 

G41 means the cutter stays to the left of the programmed path.

G42 means the cutter stays to the right of the programmed path.

 

If this is true with WEDM as well, is it not that important knowing the tolerance is pretty small so I should still get my .5 dia hole within or am I losing my case?? I know for a tool(mill) it might be more relevant(left, right)...

 

 

You are correct on the definitions. I urge you to understand offsets as they are of the utmost importance. In this case your hole would come out at .510 plus your overburn. The slug in this case would come out .500. The wrong offset will cost you tons of scrap.

[jbelle7435]

You are correct on the definitions. I urge you to understand offsets as they are of the utmost importance. In this case your hole would come out at .510 plus your overburn. The slug in this case would come out .500. The wrong offset will cost you tons of scrap.

 

Good. As being new to this, the final confirmation is fine with me.

[jbelle7435]

I actual looked into this and I don't have a compensation type : 5 choices unless I am missing something...See attachment:

 

for Control Type: Mill, Router, Lathe, Wire, Mill/Turn. No Compensation type drop down and COMP direction drop down...

[Del.]

That looks fine but in your wire contour parameters under compensation you have the choice of auto,right or left.

[jbelle7435]

That looks fine but in your wire contour parameters under compensation you have the choice of auto,right or left.

 

Ah ha. Taking the guess work out 1 post at a time. Thanks. Hope I can get this part into our WIRE EDM this week and made. It will help me become more confident with this stuff. My goal is tapered holes next.

[Del.]

Jbelle, Concentrate on the fundamentals like, Is my part drawn correctly, is my start location correct, Is my wire compensation set correctly and things like that. If not then you end up wiring out a part that looks correct but it is not. Rule number one on any expensive part or one you need done quickly. Dry Run and check to verify all those things I mentioned.

[The_kid]

listen to del on this one seriously.

[SledGeek]

^^^^^^^^^^ yep,yep. It is sooo easy to mess up on wire compared to mill or lathe. Quite simply, by the time you realize it's wrong your already cutting or done. You just can't see offsets,overburn, taper angle/direction or fourth axis forms and such like you can on a mill

 

Good luck !

[htm01]

look into a class either with your MC reseller or machine dist.

[jbelle7435]

1. Great news for making strides with this. I created my 1st actual piece with MC and the WEDM!

 

2. Now its time to make sure what I want to make is represented by the code I use!

 

One concern I ran into with the 1st piece coincidentally was about the discussion earlier in this thread about compensation. My program ran as CCW and the .5 hole came out to .520. Looking at the Code I inputted and USED for machining was G03 and G42. So the wire did travel CCW and compensated to the right. I know how to fix this and get my .5 hole would be in this case leaving the G03 the same but going from G42 to G41. Thats my next run to see a better job than the .520 but how much?? With my math (.008 Wire Dia.) if I comp. to the right I will come out 100% closer to .500 or theoretically .504.

 

Now you mentioned overburn, etc not just wire compensation how do I deal with that to make it as close to .500 or .5000(tenth) as needed. Will I have to making the hole that much smaller or are there more options to control that.

[Del.]

Jbelle,

 

Forget everything you just said there.Study the fundamentals of offsets. Lets say you are wiring out a 1.00 hole dia. and you are starting in the center. You will need to create a thread point at the center. Now select Chain as your method of cutting this. Select the thread point and then select the arc at just above the 3 o'clock position on the circle. You should see your arrows of the chain pointing up at the 12 o'clock position.This means that you are cutting the hole in a ccw direction and since you are trying to maintain the 1.00 dia you would be offset to the left or a G41 and your arc moves would be a G3 for ccw. If you chained it and the arrow was pointing towards the 6 o'clock position you would be cutting in a CW direction and your offset would be to the right or G42. BOTH will make the hole correctly, BUT ONLY IF YOU UNDERSTAND WHAT IT IS DOING. Imagine as the wire was gin around the hole and you were walking directly behind the wire.If you are trying to cut the hole and the wire was moving CCW you would be standing to the left of the hole you were trying to maintain.If you are cutting the same direction BUT want to keep a 1.000 dia slug then you would be offset to the right or G42. Your machine should automatically set the amount of the offset depending on number of passes you wish to take.

The wire machine must offset half the diameter of the wire size plus the amount of overburn.If you are cutting the 1.0 hole and going ccw with an G41 offset, your wire will move to the right and your position will be approx X .491 y0. If you use the wrong offset a G42 your wire position will be approx. .509 and you just scrapped the part. This is where dry run helps so you can verify that the offsets are correct.Your program is set to wire to center of wire so it must offset in the machine half of your wire dia. plus the amount of over burn.

[Oppiz]

If you have your Thread point in the center of your hole and your compensation direction set to auto, MC will know what side of the profile to cut too. Use verify in MC to make sure your path is on the correct side.

[jbelle7435]

Jbelle,

 

Forget everything you just said there.Study the fundamentals of offsets. Lets say you are wiring out a 1.00 hole dia. and you are starting in the center. You will need to create a thread point at the center. Now select Chain as your method of cutting this. Select the thread point and then select the arc at just above the 3 o'clock position on the circle. You should see your arrows of the chain pointing up at the 12 o'clock position.This means that you are cutting the hole in a ccw direction and since you are trying to maintain the 1.00 dia you would be offset to the left or a G41 and your arc moves would be a G3 for ccw.If you chained it and the arrow was pointing towards the 6 o'clock position you would be cutting in a CW direction and your offset would be to the right or G42. BOTH will make the hole correctly,

GOT THAT 100%

 

BUT ONLY IF YOU UNDERSTAND WHAT IT IS DOING. Imagine as the wire was gin around the hole and you were walking directly behind the wire.If you are trying to cut the hole and the wire was moving CCW you would be standing to the left of the hole you were trying to maintain.If you are cutting the same direction BUT want to keep a 1.000 dia slug then you would be offset to the right or G42.

GOT THAT 100%

 

Your machine should automatically set the amount of the offset depending on number of passes you wish to take.

Not sure by this. How many passes. Would I want to take just 1 pass? Is there a setting for this offsets besides left and right spoken about earlier?

 

The wire machine must offset half the diameter of the wire size plus the amount of overburn.If you are cutting the 1.0 hole and going ccw with an G41 offset, your wire will move to the right and your position will be approx X .491 y0. If you use the wrong offset a G42 your wire position will be approx. .509 and you just scrapped the part. This is where dry run helps so you can verify that the offsets are correct.Your program is set to wire to center of wire so it must offset in the machine half of your wire dia. plus the amount of over burn.

 

that last part is ?? to me . Even if I have my compensation(LEFT< or RIGHT) and (CW or CCW) setup properly will this solve this because it sounds like not yet based on this Radius of wire+overburn

[Del.]

Your wire machine should have the ability to set the conditions for burning. Type of material, thickness of part, flushing conditions and number of passes you wish to take. you set these in the machine although you could set them up in mastercam if you wish.The machine will set your power settings and your offset amounts.

 

Your NC program will be programmed exactly to your Geometry, but the actual numbers on the machine will be different based on your offset direction and size of offset. If you use no offsets then for a 1.00 dia hole it will come out about 1.013 Dia. because now it will not offset but cut to center of wire. That's .005/side for a .010 wire plus about .003 overburn.

[Oppiz]

although you could set them up in mastercam if you wish.The machine will set your power settings and your offset amounts.

 

Your reseller or CNC software should be able to supply with this. I've been running Mits. since 1997 and I use the power setting supplied by MC.

[Del.]

Your reseller or CNC software should be able to supply with this. I've been running Mits. since 1997 and I use the power setting supplied by MC.

 

 

Personally I have not found the benefit of doing that myself since it is so easy to do at machine.

[within a thou]

Can your machine use negative offsets? If so I would just stick with G41 and forget about G42. Now when you select your chain pretend your sitting behind the arrow as if you were in a car. A positive offset will move you to the right (plus stock) a negative to the left (less stock). And Del I have to agree with you on that one if your machine automatically adjusts for the over burn why would someone want to use a third party product to over ride what the machine was designed to do?

[Oppiz]

Personally I have not found the benefit of doing that myself since it is so easy to do at machine.

 

I guess it's matter what you're used to. I have been using the new "Tech" style of power settings some. It works pretty good most of the time. All you do it input material thickness, wire dia. and surface finish and it outputs the correct amount cuts,offsets and power settings.

[Del.]

I guess it's matter what you're used to. I have been using the new "Tech" style of power settings some. It works pretty good most of the time. All you do it input material thickness, wire dia. and surface finish and it outputs the correct amount cuts,offsets and power settings.

 

 

Yeah, If it is set correctly I think it would be fine. It just seemed like too much work to me and the last thing I want is someone else doing it who know nothing about the fundamentals of WEDM.

[FROZEN]

You need to take in account for finish. If your just dropping a slug ±.002 depending on material. You should be taking a finish pass at a little power setting to get better finish to hold ±.0002.

[jbelle7435]

You need to take in account for finish. If your just dropping a slug ±.002 depending on material. You should be taking a finish pass at a little power setting to get better finish to hold ±.0002.

 

This what I learned around closing time after I coded the CCW with the G41 command. Now I am on the small "safe" side I can work my way to the tight .5000 tol and +/-.0002 is in the ball park I need! Trial and error work better with more knowledge added each time